Defining a point PT in an Apt programming

                        In NC Programming the APT programs plays a major role, the geometries are defined by APT programming and then converted into G-codes giving motions to the CNC machine.

  Defining a point in the APT programming, the statement used is GOTO/P1; the programmer must know where P1 is located before the statement can be effective. P1 therefore must be described in a geometry statement, prior to its use in the motion statement GOTO/P1.

The geometry statement for defining a point is P1 =POINT/X co-ordinate, Y co-ordinate and Z  co-ordinate where, P1 is known as a symbol Any combination of letters and numbers may be used as a symbol providing the total does not exceed six characters and at least one of them is a letter.If the Z co-ordinate is zero and the point lies on the XY plane, the Z location need not be noted.Here “PT’ is a POINT. This word is a vocabulary word. Throughout, the designers of APT have tried to use words that are as close to English as possible. A slashfollows the vocabulary word and is followed by a specific description of the particular geometry, such as the coordinates of the point P1. AnAPT programming statement for P1 might appear as P1 = POINT/1, 5, 4. The 1 would be the X ordinate; the 5, the Y ordinate; and the 4, the Z ordinate. Lines

Examples for the Point definition in APT programming:

There are other ways of defining the position of a point, such as at the intersection of two lines or where a line is tangent to a circular, intersection of two circles, single point in space etc. following pictures shows the different ways of defining the Point in an APT programming.

Point in Space: Any point in the space can be defined as shown below.

APTSource code:
P1=POINT/4,5,2
P2=POINT/2,2






------------------------------------------------------------------------------------------------------------

Intersection of two lines: Point can be created by intersection of two lines.

APTSource code:
P1=POINT/INTOF, L1,L2













--------------------------------------------------------------------------------------------------------



Intersection of two lines: Point can be created by intersection of line and circle. there are two possibilities, it can be written as below.

APTSource code:

P1=POINT/XLARGE,INTOF,L1,C1
                       OR
P1=POINT/YLARGE,INTOF,L1,C1
---------------------------------------
P2=POINT/XSMALL,INTOF,L1,C1
                       OR
P2=POINT/YSMALL,INTOF,L1,C1

Note: The X and Y co-ordinates of P1 is Larger than the X and Y co-ordinates of P2.


------------------------------------------------------------------------------------------------------------


Intersection of two Cirlces: Point can be created by intersection of circles. there are two possibilities, it can be written as below.

APTSource code:
P1=POINT/XSMALL,INTOF,C1,C2
                         OR
P1=POINT/YLARGE,INTOF,C1,C2
---------------------------------------
P2=POINT/XLARGE,INTOF,C1,C2
                         OR
P2=POINT/YSMALL,INTOF,C1,C2

------------------------------------------------------------------------------------------------------------

Intersection of a radial line and a circle: Point can be created by intersection of circle with a radial line can be written as follows.

APTSource code:
P1=POINT/C1,ATANGL,20

------------------------------------------------------------------------------------------------------------

Intersection of a radial line and a circle: Point can be created by intersection of circle with a radial line can be written as follows

APTSource code:
P1=POINT/CENTER,C1










This is how the APT codes can be written in APT programming. All software generates the APTSource fiiles using the PPtables used while generating. PPTables are the machine defined files where all the cycles and the movements are in machining standardized format

G28 Return Home

G-Code G28 Return home:

G28 Is the G-Code that instructs the Controller of the machine to move the tool automatically to the reference point.  The Reference point is the fixed position on the machine, to which the tool can be moved.  This reference point is also called the “Home position”. Machine has the reference point for  X, Y and Z Axis.

G28 G-Code Format:

N170 G90 G28 X_ Y_ Z_; (Absolute Code)
Or
N170 G91 G28 X_ Y_ Z_; (Incremental Code)
                    Where X, Y and Z can be used to indicate an intermediate point, through which the tool will pass, before continuing to the reference point.  If the intermediate point is not set, tool may move in non-vector type path.  It may collide with the part or the fixture, so you can put the intermediate values in X, Y and Z to move the tool first to safety plane.
                     The move to any intermediate point and the reference point are performed at a rapid traverse rate.

Example Below shows the collision scenario 1:

 The diagram below shows how the tool could collide with the billet when moving towards the reference point with Non-vector type movement.

To avoid this collision, the tool is sent on a path which includes intermediate point P2. The intermediate point is used to allow the tool to move completely clear from the billet, before continuing onto the reference point, P3.

The above tool path can be programmed as follows (In absolute mode, G9Ø):

G90 G28 X60 Z60;

The above tool path can be programmed as follows (In incremental mode, G91):

G91 G28 X0 Z40;

So that the Tool moves to the safety plane before it reaches the Reference Point.

Example Below shows the collision scenario 2:

In the diagram below, the tool is in a position (P1) where there is no obstacle to collide. The intermediate point, in this case, is not required, so the block can be written as follows:

(In incremental mode, G91): G91 G28 X0 Y0 Z0; 

NOTE :  G28 is a non-modal G code. It is only active in the block in which it is programmed.

NOTE: If no X, Y, Z, or A is specified, all axes will be moved directly to machine zero. Any auxiliary axes (B, C...) are returned to the machine home after the X, Y, Z, and A axes. G28 will not recognize any tool length offsets in this move.